Fullscreen HTML5Med Res (??MB)HTML4

HOW TO DESIGN Printed Circuit Boards Part 3 by Tim Blythman Getting PCBs made is quite cheap these days, and as we have explained in the first two parts of this series, EDA (electronic design automation) software is powerful and easy to use. This final article in the series looks at some of the advanced options and techniques that you might use to design your own PCBs. We’ll also cover what’s required to get entire PCB assemblies made. I n the first part of this series on How to Design Printed Circuit Boards, we described the basics of setting up symbol and footprint libraries to streamline the PCB design process in Altium Designer (most other EDA packages have similar workflows). We also explained how a manufacturer takes the Gerber files and turns them into a completed PCB. In Part 2, we walked through the steps of laying out a schematic (circuit diagram) and then transferring that to the PCB editor to allow components, traces and other features to be arranged to complete the board. We offered a few tips and tricks along the way. The most recent article finished with instructions on how to use exported “Gerber” files to order from a manufacturer like PCBWay. The number of options is incredible, as you 70 Silicon Chip would have seen in Fig.20. While the defaults are suitable for a vast majority of designs, we will next delve into some of the more interesting and useful options. This article will then investigate some of the requirements for PCB designs that involve high voltages, high currents or high-speed signals. That will include how to approach these concepts at the design stage, and how some of the specialised PCB purchasing options can address concerns relating to advanced designs. As you would have seen from project articles such as the RP2350B Computer (November 2025; siliconchip. au/Article/19220) and the RGB LED Star (December 2025; siliconchip. au/­Article/19372), it is now possible (easy, even) to design and order complete, custom PCB assemblies (PCBAs). Australia's electronics magazine A PCBA is simply a PCB that has been fully or partially populated with components. In cases like the RP2350B Computer, that means that you could receive a practically completed project; perhaps needing little more than a case. So this article will also discuss what is needed to design and order a PCBA. More PCB options Some of these options are fairly obvious, while others are a bit obscure, and their cost can vary markedly. Fortunately, manufacturers like PCBWay automatically update their pricing based on selected board options, so you can easily see what specific combinations of options might cost. In Fig.20, you can also see the small “?” icons that provide further detail on how some of these options work. We’ll discuss some of the more interesting options below. The board type option allows the PCB to be manufactured in larger panels consisting of more than one board. There is little advantage in this if you are ordering just a few PCBs. The larger panels are easier to handle if there are further automated processing steps that need to happen, such as being fitted with components to create a PCBA. These panels make for easier processing in the pick-andplace machine and reflow oven. When you upload Gerber files at the start of the ordering process, the size will be automatically detected, but you can manually enter a figure to see how the cost changes for different sizes. Keep in mind that the size really refers to a rectangle that contains the entire PCB shape, so an unusual shape might benefit from being rotated to minimise its dimensions. A good example of how this works is the RGB LED Star. Hanging in its obvious orientation (with the long arms vertical and horizontal), a PCB manufacturer would measure it as 240mm × 240mm. By rotating the design by 45° within Altium Designer, this is reduced to 170mm × 170mm, which ends up being much cheaper to manufacture. You can see this in Fig.21. For a prototype, you might only need a single board, but five is the usual minimum order quantity (MOQ). It just isn’t worthwhile for the manufacturer to make fewer than that. Five small double-sided boards can siliconchip.com.au be surprisingly cheap to order (a few dollars plus postage). Advanced options We are now getting into some of the more advanced (which can mean expensive) options. Multi-layer boards (with more than two layers) have certainly become cheaper, and will often be necessary for high-speed designs. Four-layer boards are commonplace. Manufacturers no longer offer discounts for single-sided designs except in huge quantities; two layers is generally the minimum practical number. The material option refers to the substrate; FR-4 glass-epoxy laminate (fibreglass) is widely used and well characterised, so it is easily the cheapest. Aluminium-cored PCBs are not too expensive for single-layer designs, and would be chosen for their improved thermal conductivity over FR-4 in high-power designs like LED lamps. However, they can be difficult to solder by hand; a reflow process is generally required. PCBWay offers flexible PCBs (www. pcbway.com/flexible.aspx), these are reasonably priced for small designs; we used a flexible PCB as a slim interboard connector in the USB-C Power Monitor (August & September 2025, siliconchip.au/Series/445). So they are worth considering where you need a board or cable that can bend. Some simulation features in Altium Designer can depend on the dielectric characteristics of the substrate, so if you are planning to use a different substrate, be sure to update the Layer Stackup to suit. The impedance of differential pairs also depends on the substrate characteristics, so you will need to check this if you are routing high-speed differential pairs. A typical PCB is 1.6mm thick, but for a two-layer board, you can reduce the thickness to 1.2mm, 1.0mm or 0.8mm without increasing the cost. Thinner boards are available but are more expensive and less robust. For panels, a slimmer PCB will often be more elegant. Some components, like the USB plugs that we used in the USB-C Power Monitor, require a specific board thickness, so you might find that your components dictate this option. The default options for minimum hole size, track width and spacing should be fine for most hand-soldered siliconchip.com.au Fig.20: PCBWay offers many options for its PCB manufacturing service; there are other tabs offering advanced options and flexible PCBs as well. To see the full range of options, visit www.pcbway.com/orderonline.aspx Fig.21: our RGB Star looks best hanging vertically, but designing it like this (or at least rotating it before fabrication) allows it to be made much more cheaply. Australia's electronics magazine February 2026  71 Fig.22: this ruler is actually a PCB that has been designed by PCBWay to show off their multi-coloured PCB printing capabilities. designs. If tighter tolerances are needed, they may be available for an extra charge, since the processes need to be more exacting. If your design uses BGA-packaged chips or other finepitch parts, you might need to check these parameters when setting up your design rules. In our experience, the different solder mask and silkscreen colours do not add extra cost, but anything different to white silkscreen printing on a green solder mask will take longer to produce. So we generally stick to that unless there is a good reason to use something different, such as using a black solder mask for panels so that they match the rest of the enclosure. The PCB colour can also be chosen for aesthetic purposes, such as the red PCB used in the FlexiDice (November 2024; siliconchip.au/Article/17022). Note that while black and white PCBs look nice in certain applications, it can be hard to see the tracks under those solder mask colours, which may make debugging harder. Multi-colour printing Multi-colour printing on PCBs has recently become available; the printing applies to the silkscreen layer. This process uses UV-reactive inks that are similar to those used for traditional silkscreens and solder masks, except they are capable of reproducing a full range of colours. Fig.22 shows a sample of a PCB that has been produced using this process. The process is analogous to CMYK printing on white paper, so a white solder mask is required as the base to give the best results. PCBWay provides a guide to their process at siliconchip. au/link/ac9g Since the Gerber format has no way to handle this colour information, the process involves creating image files (JPG etc) for the top, bottom or both layers. A third image can be provided as a reference to show how the images should be aligned to the PCB. with a suitable receptacle. Various types of computer cards are probably the best-known examples; hence, they are also known as card-edge connectors. Modern PCI Express cards still use the same principle as the original IBM PC from the 1980s. Figs.23 & 24 show a typical edge connector and a matching receptacle. While they look deceptively simple, edge connectors require extra PCB processing steps for correct operation. They should have a hard gold plating to give the necessary durability to the contact surfaces. The edge should be given a bevel to ease its insertion into the connector; all these steps add extra cost. Surface finish There is also the option to choose a surface finish for the exposed copper on the board; that is, the copper that is not covered by solder mask, which mainly means component pads. We mentioned some of the options in the Part 1 panel on the PCB manufacturing process. These finishes are intended to protect the pads from corrosion until they are soldered to. For cost reasons, we practically always choose the HASL (hot air solder level) process; this coats the copper with a thin layer of solder. Interestingly, the process for flexible PCBs requires a gold finish such as ENIG, since the tin-based solder used in the HASL process does not handle flexing well. Other options include OSP, which stands for organic solderability preservative, a coating that is dissolved during the soldering process. ENEPIG adds a durable palladium An edge connector is made of traces on the PCB that end in fingers that mate Fig.23: this PCIe receptacle is typical of the type that allows an edge connector to plug in. Source: Mouser 571-5-1734857-5 72 Australia's electronics magazine Edge connectors Silicon Chip layer between the nickel and gold of the ENIG process. The silver and tin immersion finishes use a chemical (non-electrolytic) plating process to add thin layers of their respective metals to the copper for protection. These are not as resistant to oxidation as HASL, but this is not a concern where the boards are populated soon after manufacture, such as when you’re using a PCBA service. Plugged vias are more expensive than plain vias. In this case, the empty space of the via hole is filled with resin to provide a flat surface at each end. This is only necessary in cases such as where there is a via in a pad and the PCB is assembled with a reflow process, although it also reduces the chance of via corrosion later, especially for larger vias that can’t be tented. You can designate uncovered (untented) vias by having openings in the silkscreen, but the best practice is usually to leave them covered, since that will leave them less exposed to oxidation or inadvertent contact. Production code You might have seen that our PCBs have a code printed on their silkscreen layer that does not match the eightdigit PCB code that is printed elsewhere. This is a tracking code used by the PCB manufacturer during the production and is selected at the “Remove product No.” option. This is needed because many PCB orders are combined into a much larger panel during production. When Fig.24: an edge connector has goldplated fingers to mate with the connector shown in Fig.23. Source: PCBWay – siliconchip.au/link/ac9j siliconchip.com.au the panel is separated, the individual PCBs need to be identified and sorted. Removing the tracking code entirely will cost extra, since the PCBs need to be identified another way. It’s also possible to add specific text (eg, “WayWayWay” for PCBWay) to one of the silkscreen layers to mark a desired location for the code. This means that the marker text will be replaced by the tracking code in the finished PCB. The above covers many options, many more than we have ever used. For the curious, there is also an advanced tab, with even more options! High-current designs Last month, we noted that many simple designs can be completed without worrying about requirements related to high currents, high voltages, high-speed signals or RF. The main option in PCB manufacture that relates to high-current design is copper thickness. The standard copper thickness on FR-4 PCBs is one ounce per square foot, which you will see quoted as “1oz copper”. Based on the density of copper metal, this is nominally 0.035mm (35 microns or 35μm) thick. You might choose thicker copper to reduce resistance in a high-­current or high-power design; the aim is to reduce dissipation through ohmic (resistive) losses in the traces. We have used 2oz (70μm) copper in a handful of high-current designs, most recently the Ideal Diode Bridge Rectifiers (December 2023; siliconchip.au/ Article/16043). Much heavier copper layers are possible; Fig.25 shows an example of a PCB with 20oz (0.7mm-thick) traces! The thickness is made by plating extra copper onto the existing copper, which means that extra copper must also be etched away in places. The PCB Assembly Pitfalls While it’s certainly tempting to get someone else to assemble boards for you, the process is not without its hazards. Two problems we’ve experienced so far are: #1 Defective parts: prototypes of the Pico 2 Computer (April 2025 issue; siliconchip.au/Article/17939) worked fine. The ‘production’ batch of boards unfortunately didn’t due to a different batch of CH334F USB hub ICs being used, which were faulty. Luckily we just needed to remove two resistors from the board, bypassing the faulty function, allowing the boards to work. But the chips could easily have had a flaw that wasn’t fixable without replacing them, and they’re QFN chips – not easy to replace! #2 Incorrect assembly: we quadruple-checked the orientation of the small yellow SMA tantalum capacitor shown in the photo below before ordering the boards. On receiving them, when power was applied, too much current was drawn. We realised that the tantalum capacitors had been installed backwards. The right-hand photo shows the preview on the JLCPCB website. When we queried it, they told us that the preview is not 100% accurate and that we need to request to be sent images to check before manufacturing starts. Again, this was fixable, but time-consuming. Still, we think they should have alerted us that the manufacturing plan differed from the preview. The yellow/orange SMA tantalum 22μF capacitor shown in the left-hand photo was installed backwards compared to the adjacent preview image. deeper etching requires tighter controls to achieve the same outcome as 1oz copper. The etched copper also adds to the amount of dissolved copper that must be handled as a waste stream of the process. For these reasons, it’s often cheaper and quicker to design wider traces with 1oz copper in mind. Also Fig.25: this board for a Formula E electric race car costs over $2000. It has extremely thick tracks for high current handling and spacing for voltage separation. Source: PCBWay siliconchip.au/ link/ac9k siliconchip.com.au Australia's electronics magazine consider that at higher frequencies, the skin effect makes thicker traces less effective. The copper layers can also be enhanced with manual post-processing. For the Versatile Battery Checker (May 2025; siliconchip.au/Article/18121), we removed the solder mask above some of the high current traces, allowing them to be supplemented by adding solder during the construction phase. This is a trick that many manufacturers use as it’s cheap if done sparingly. Design rules review Now we will look more closely at some factors that might complicate designs involving high currents, high voltages, high-speed signals or RF. It’s a good idea to have experience with these sorts of concepts before attempting to design PCBs with them. February 2026  73 In these cases, there are design rules that can be applied to ensure that the necessary requirements are met. The design rules won’t guarantee perfect results, especially when the PCB exists in a real world with unpredictable external conditions, but they will help. For high-current designs, the trace width is typically the most critical parameter. Copper has a finite resistivity, typically given as 1.7×10-8Wm at room temperature. The units of Wm mean that you can get a resistance (in ohms) by multiplying by the length and dividing by the cross-sectional area. On a 1oz PCB, this means that a trace 1m long and 1mm wide has a resistance of around 0.5W. That on its own does not tell you how wide a trace should be, so the IPC-2221 standard has been developed to formalise good practice. Altium Designer has a built-in resistance calculation tool in its PCB editor as well as an online guide and calculator for this aspect of IPC-2221 at siliconchip. au/link/ac9h These calculations are based on the expected rise above ambient temperature due to ohmic heating, and are simplified with a number of assumptions; for example, the ability for internal layers (on a multi-layer PCB) to shed heat is much reduced compared to external layers. A good working figure is a 10°C rise, and even then, IPC-2221 is considered quite conservative, since it does not take into account other nearby traces and copper areas. IPC-2152 is another standard that considers even more factors. Thus, it’s a good idea to set up a design rule that ensures that all the traces are wide enough for the current they will carry. Since you don’t need all traces to be subject to the same width rules, Altium Designer also includes the concept of net classes to selectively apply different design rules. We can also use net classes in high-voltage, high-speed and RF design. Net classes While it is possible to create a net class in the PCB Editor, it’s best to do so from within the Schematic Editor. Here, the nets correspond to wire objects, so we simply need a way of marking each wire object with its desired net classes. This is done by placing a Parameter Set object (Place → Directives → Parameter Set). The Parameter Set object can be used to set much more than just net class. It is attached to the wire and needs to have a net class added. The net class name is set with a string (such as “POWER”), and its label can be set so that its purpose on the schematic is clear. The Parameter Set object can now be copied and pasted as needed to add other wires to the same net class. Fig.26 shows a design with several POWER net class objects. The net classes are carried through with the nets into the PCB design (when Update PCB Document is performed); thus, the traces for those nets will also belong to the net class. The next part of using net classes is to create custom rules that apply to them, such as a minimum trace width rule for current handling. Fig.27 shows the updated design rules in this case. Fig.26 (below): adding a Parameter Set object allows wires (and thus the resulting nets and also the traces in the final PCB) to be assigned to a net class to allow specific design rules to be applied. Fig.27 (left): this custom rule applies to members of the net class and enforces a minimum width. Fig.28 (lower left): during routing, a trace is flagged if it does not meet the width specification for its net class. 74 Silicon Chip Australia's electronics magazine siliconchip.com.au Fig.29: the Layer Stackup Manager is used to enter the properties of the PCB stackup, such as layer thicknesses and dielectric properties. Among other things, this allows an impedance profile to be created. Fig.30: the impedance profile is used as the basis of a design rule to enforce the trace width and spacing to maintain the impedance of the differential pair. A second routing width rule (that we have called Width_POWER) has been added. It is applied to the POWER net class by using the dropdown menus to select the correct object matching criteria. Its priority has been set to overrule the default rule (when it is applicable) and the minimum width increased to an appropriate value. Fig.28 shows the result of this rule being applied to a trace in that net class. When the trace is reduced below the minimum width, it is flagged as a design rule violation. Another, thinner trace is not flagged, since it is not a member of the POWER net class. High voltages The most obvious design rule for high-voltage design is clearance, which is the spacing between traces on the same layer. Altium Designer can also apply a design rule for creepage, which tests the distance between traces along the board surface and can take account paths through holes, cutouts and even around the edge of the board. The way to enforce clearance for high-voltage traces is to use the Parameter Set method to create a high-voltage net class and then create an appropriate design rule invoking that net class. Since clearance and creepage rules involve two traces, there are two dropdown menu options to be selected. One should be the relevant net class, while the other should be “All” to ensure that clearance and creepage are maintained to all other copper. It’s possible to set a net to be part of multiple classes if needed. siliconchip.com.au Creepage is also affected by the substrate thickness, so the Layer Stackup becomes important, since it will dictate the board thickness and thus the length of the creepage path. The PCB thickness is used in the IPC-2152 PCB trace width calculations. It is critical in high-speed design, especially since dielectric characteristics will affect signal propagation. High-speed signals High-speed and RF PCB design is a very broad topic. There isn’t necessarily a fixed point at which a PCB becomes high-speed; it is related to when the traces behave more like transmission lines than simple wires, so concepts like trace impedance become important. It’s imperative to use the Layer Stack Manager (under the Design menu in the PCB Editor) to make sure the settings match the intended PCB manufacturing process and materials if high-speed signals are involved. Fig.29 shows the Layer Stack Manager with the Impedance tab opened. With an impedance profile set, it becomes available as a design rule, and can be applied to traces in the same fashion we have discussed for other net classes. Single conductor Australia's electronics magazine and differential pair (Fig.30) impedance profiles can be set. Altium Designer can also provide calculations and simulations, so it’s possible to check and validate a design after it has been routed and before it is manufactured. PCB design is an iterative process, so don’t be surprised if you need to go back at some point and rework your layout. One important factor in high-speed design is that if you have multiple related signals (eg, a parallel memory bus or a differential pair), the track lengths should be as close to identical as possible so the signals arrive at the same time. Altium and other ECAD packages provide tools to help ensure this is the case. Minimising magnetic loops (eg, through the use of a ground plane) is also important, as is considering the effect of crosstalk between adjacent or nearby high-speed conductors. PCB assembly Some PCB manufacturers now offer PCB assembly (PCBA) services. This involves having the PCB made, then populated with components. We have done this now for a handful of projects where it would be difficult to hand-­ solder the necessary components, such as the QFN-80 package RP2350B chip. February 2026  75 Since JLCPCB was quick to offer the RP2350B chips, we used their PCBA service for two RP2350B-based projects. We also used them for the RGB LED Star, since we were familiar with their requirements and process. Fig.31 shows the Star assembly that we received from JLCPCB. Different PCBA manufacturers offer different ranges and sources of components. So we suggest picking a company before performing schematic capture, as you will need to know what components and variants are available in sufficient quantities before commencing layout of your design. JLC’s low-cost service is well-suited to simple designs, while PCBWay offers considerably more flexibility, so they are generally recommended for assembling more advanced designs. For example, JLC doesn’t offer blind or buried vias, which are required for many PCB designs that include BGA (ball grid array) package parts. Overview The process we’ll describe for designing and ordering PCBAs applies to JLCPCB’s service. It should be fairly similar for other manufacturers like PCBWay, but we recommend checking their specific requirements before starting a design. In addition to the Gerbers needed for making the PCB, you’ll need a bill of materials (BOM) and a component placement list (CPL) files. The latter might also be known as a ‘pick-andplace’ file; it is mainly a list of the components and their locations and orientations on the board. Both of these are simply spreadsheet files in Microsoft Excel (XLSX) format. Other spreadsheet formats, such as comma separated value (CSV), are also supported, so you can view and edit them using free software such as LibreOffice (which also supports the XLS/XLSX file formats). Altium Designer can export these files, but there is specific information that needs to be entered to ensure that the correct data is available. This includes things like component part numbers and suppliers, which will be specific to a PCBA manufacturer. The PCB ordering process happens as usual and is followed by an option to enable PCB assembly. This step will require the BOM and CPL files to be uploaded. Then there are selections related to the assembly process that will need to be made. Let’s start by looking at what needs to happen in Altium Designer. In Part 1, we provided a panel detailing how PCBWay takes the Gerber files and turns them into a PCB. The panel opposite describes how the BOM and CPL files are used to assemble the PCB and components into a PCBA. Schematic capture changes During the schematic capture, each component needs to have information added to indicate its supplier and part number. There are added as Parameters in the component properties, as seen in Fig.32. The Supplier and Supplier Part fields are required, but we have added the other fields for completeness. LCSC (www.lcsc.com) is a sister company of JLCPCB, and the part numbers are the same as JLCPCB’s (https://jlcpcb.com/ parts). It’s possible to source parts from other distributors, although we have not needed to do this. These parameters will be carried over if the parts are copied and pasted during schematic capture. Where possible, use the Basic parts type. Extended parts are more expensive to use, since they will need to be manually loaded into the pick-and-place machines before they can be installed on the PCB. You can filter by type in JLCPCB’s parts search. For example, this means that it’s considerably cheaper to use M2012/0805size passives or smaller, as they are Basic parts, while M3216/1206-size parts are mostly Extended. Remember, you don’t need to solder these parts – they will be doing it for you! Of course, you want to make sure that the parts have ample stock; we would expect that the Basic parts would be maintained in stock, since they are always loaded in the pick and place machines. (JLCPCB lets you preorder parts to ensure they’re in stock when you’re ready for assembly, but we won’t explain that process here.) Broadly speaking, the design will be cheaper to manufacture if you can minimise the number of different part numbers that are used, since there will be fewer parts that need to be loaded into the pick and place machines, and you will get better quantity discounts. It will also be less work to source substitutes if needed. This is just a small part of the larger field known as design for manufacture (DFM). Fig.31: RGB LED Stars are received by us attached to PCB rails that have fiducial (locating) marks to assist their processing during assembly. Fig.32: adding these parameters to each component during schematic capture ensures they are linked to the correct inventory part for the assembly stage. 76 Australia's electronics magazine siliconchip.com.au The PCB assembly process We explained in Part 1 of this series (December 2025 issue; siliconchip.au/ Article/19373) how Gerber files are turned into a PCB. Now, we will look at the processes involved with populating that PCB with parts as might be done by a typical PCBA provider. For boards with just surface-mounted parts, there are four main steps. First, the boards have solder paste applied to the pads where needed. Then the components are placed onto the PCB by pick-and-place machines. The components are soldered by passing the board through a reflow oven, after which a final inspection occurs. Through-hole parts are often still manually fitted and soldered, although some can be placed by machine, with the board being soldered by a wave-­ soldering process that rides the board over a bath of molten solder. We’ll focus on the surface-mounting process, since we expect most readers will be interested in that aspect. You can see from Fig.31 in the main article that the PCBs for our RGB LED Star are fitted with rails along the edges. These rails have markers so that the various processes work to the same alignment. The rails also make it easier for the boards to be transported through and along the steps in the process. Solder paste To apply the solder, a laser-cut stainless steel stencil is produced. The thickness of the steel, combined with the size of the holes, determines how much solder is applied. It is applied with a squeegee that forces the solder down onto the PCB through the holes in the board. PCBWay uses an automated camera-­ based inspection process to verify the process. Differently coloured lights are shone from different angles to allow the height and location of the applied solder paste to be checked. The YouTube video at https://youtu. be/24ehoo6RX8w shows a tour of PCBWay’s assembly factory in Shenzhen, Fig.c: the boards enter the reflow oven for soldering. Source: https://youtu. be/24ehoo6RX8w siliconchip.com.au Fig.a: solder paste application using an automated stencilling machine. Source: https://youtu.be/24ehoo6RX8w Fig.b: components are picked up from the reel at the front & placed on the PCB. Source: https://youtu.be/24ehoo6RX8w China by Scotty of Strange Parts. Fig.a is a still from this video and shows the automated stencil applying the solder paste to a board. from April and May 2020 implements this same process (siliconchip.au/ Series/343). Since the factory is more like an assembly line, the reflow oven is a long machine, with the temperature profile being achieved by different temperature zones along the machine’s length. Fig.c shows the boards entering the reflow oven. The solder paste is a suspension of small balls of solder in flux paste, so when the appropriate temperature is reached, the solder melts and the flux is activated, soldering the component to its pads. Pick-and-place The BOM file is used to determine which parts are loaded into the pick-andplace machines. Fig.b shows one of the machines in operation. In the processing line shown in the video, the board actually passes through three pick-and-place machines in succession. The machines take components one at a time from a reel using a small vacuum head. They then place them on the board, where they loosely adhere to the solder paste. The machines in PCBWay’s factory are also fitted with cameras. One camera is used to register the markers to know where the board is. Another camera observes each component after it is picked up, and the computer can determine how much the part needs to be moved or rotated to get it in the correct position. There is another inspection stage after this; an operator can move any components that are not where they should be before the next stage. Reflow The reflow soldering process demands an exacting temperature profile to achieve optimal results. The temperature is slowly ramped up to the target and is then held for a time before being allowed to decrease. Our Reflow Oven Controller Fig.d: automated inspection uses coloured lights to highlight defects. Source: https:// youtu.be/24ehoo6RX8w Australia's electronics magazine Inspection The completed board is inspected with a similar camera to that used for the solder paste. Fig.d shows a view from the computer that processes the inspection. Differently coloured lights are projected at different angles and strike the components and solder fillets in distinctive patterns. The patterns are compared to a board that has been manually inspected and validated. If necessary, components are marked for rework, which is done manually. BGA (ball grid array) chips don’t have any visible pins, since they are all under the body of the part. These can be inspected by an X-ray machine. Summary These are just the main steps involved in PCB assembly. Double-sided boards can be made with these processes, but usually require the components on one side to be secured with glue, so that the board can be inverted to process the other side. There are optional post-processing steps that can be done, such as programming, functional testing and conformal coating. But it’s incredible to think that it’s now possible to design your own project and have it be fully assembled and delivered to your door at a price that hobbyists can afford! February 2026  77 PCB export Fig.33: after the CPL file is exported here, it may need some editing to ensure that it conforms to the format expected by JLCPCB. The new parameters are carried over to the PCB layout stage, and can be viewed there, but there isn’t anything else that needs to be done during layout until the design is finalised and exported for manufacture. After exporting the Gerber files in the usual fashion, use File → Assembly Outputs → Generate pick and place files. Fig.33 shows this screen. Ensure Metric units and Show Units are selected and export to CSV format. Find the Project Outputs subdirectory where your project is saved. You will see a CSV file that you can open in LibreOffice Calc, Microsoft Excel or similar. The first 12 or so rows are not useful to us, so delete them, moving the column headings up to the first row. Next, we need to change some column names as they are not what JLCPCB is expecting. Change the “Center-­X(mm)” heading to “Mid X” and the “Center-Y(mm)” heading to “Mid Y”, then save it as an XLS file. This will be your CPL (component placement list) file. To generate the BOM, click Reports → Bill of Materials. On the right side of the dialog that appears, under Properties, click Columns and then make sure your parameter columns are visible (click the grey eyes to turn them white). Go back to the General tab and under File Format, select “Generic XLS”, then click the Export button at lower right. Manufacturing Figs.34 & 35: the RP2350B Development Board uses tiny SMD passives and a QFN chip. It would be quite difficult to hand-solder, so it’s handy to be able to get this board fully assembled. It is a simple design with components on one side. Thus, it qualifies for the Economic manufacture option. Let’s work through the ordering process using the files for the RP2350B Development Board. The board is shown in Fig.34. You can follow along by downloading the required files from siliconchip.au/Shop/10/2832 Start by uploading the Gerber file (with the ZIP extension) as you would for any other PCB design. Validate that the Gerber is correct and make any selections as necessary for the PCB. Scroll down the page and turn on the switch for PCB Assembly, which will pop out some related options, which you can see in Fig.35. Economic PCB assembly is possible for this board, since it is an uncomplicated design with components on just one side, and the remaining options can be left as their defaults (you may want to select the Board Cleaning option to remove residue as it costs Australia's electronics magazine siliconchip.com.au 78 Silicon Chip Fig.36: on this page, you can opt to leave components off or select substitutes if your preferred part is unavailable. Fig.37: the Component Placements page allows the position and orientation of the components to be checked & adjusted if needed. Note the purple dot indicating pin 1 on the polarised components (but you can’t always rely on this). little). There is a comprehensive list of the different assembly types at siliconchip.au/link/ac9i Interestingly, we had to use the Bake Components option for the RGB LED Stars, since the WS2812B RGB LEDs are highly susceptible to absorbing moisture. This can lead to the evocatively named ‘popcorning failure’ when the parts are heated during reflow soldering. We also had to select the Standard PCBA type for the RGB LED Stars, since these PCBs have components on both sides. Click Next to proceed; the next page is simply a PCB viewer, so you can click Next again if the PCB looks correct. This page allows you to upload the BOM and CPL files, after which you should click Process BOM & CPL, which leads to the screen seen in Fig.36. This page allows you to check and confirm that the listed components are able to be matched. If they are not, you can use the search button to find an alternative. Any parts that do not have a blue tick in the Select column will not be fitted, so you can use this page to deselect any parts you don’t want fitted. The Lib Type column shows that the Basic parts are mostly passive components with common values. After clicking Next, you might see a warning about using a non-standard power supply configuration for the RP2350 IC; this is fine to click through, since this is a proven design. Our RP2350B Development Board article explains the configuration. 🔍 siliconchip.com.au Fig.37 shows a simulated view of the board with all the components in place. Here, you can check and edit the orientations and locations of the components. You can see that polarised components have a purple dot marking pin 1. You can match this to the pin 1 silkscreen marker to confirm the orientation. If anything is wrong, there are buttons to move and rotate the parts. You can also click on the image or list to select and highlight certain parts before editing them. If there are problems, it is a good idea to go back to your design and edit the components to ensure that future designs do not have such problems. Click Next when you have checked all the components on this page. Fig.38 shows the final breakdown of the costs for board manufacture and assembly (in USD). There is an item for a stencil, but it’s interesting to note that you do not need to provide paste mask files (for the stencils). The paste masks and stencils are generated by JLCPCB. The components are the largest cost, but the fee for using extended components does make up nearly 1/3 of the total. To complete the order, select Save To Cart and complete the order as you would for any other online shop. As you would have seen from the RGB LED Star, there is no requirement that all parts be fitted. In the same vein, it’s not necessary to have all boards assembled either. You could order five boards and only have two boards assembled (the minimum number), which would save on parts and Australia's electronics magazine assembly costs if the design is only at the prototype stage. Summary PCB (and PCBA) design is a broad field, and we cannot hope to cover all the factors that influence the journey from concept to completed project. We hope that the information we have provided in this series is helpful in producing your design. If in doubt, simply try making your own PCBs if you have not done so already! The Altium Academy YouTube channel has numerous tutorials on PCB design using Altium Designer (www. youtube.com/<at>AltiumAcademy). SC Fig.38: the final cost breakdown shows how much of the total is due to the use of Extended components. So it’s a good idea to use Basic parts if possible. February 2026  79